This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

1 

Proceedings of the 2008 ASME Rail Transportation Division Fall Technical Conference 

RTDF2008 

September 24-25, 2008, Chicago, Illinois, USA 

RTDF2008-74022 

FINITE ELEMENT ANALYSES OF RAILROAD TANK CAR HEAD IMPACTS 

Y.H. Tang 

Volpe National Transportation Systems Center 

Cambridge, Massachusetts, USA 

H. Yu 

Chenga Advanced Solutions & Engineering, LLC 

Cambridge, Massachusetts, USA 

J.E. Gordon 

Volpe National Transportation Systems Center 

Cambridge, Massachusetts, USA 

D.Y. Jeong 

Volpe National Transportation Systems Center 

Cambridge, Massachusetts, USA 

ABSTRACT 

This paper describes engineering analyses of a railroad 

tank car impacted at its head by a rigid punch. This type of 

collision, referred to as a head impact, is examined using 

dynamic, nonlinear finite element analysis (FEA). 

Commercial software packages ABAQUS and LS-DYNA are 

used to carry out the nonlinear FEA. The sloshing response of 

fluid and coupled dynamic behavior between the fluid inside 

the tank car and the tank structure are characterized in the 

model using both Lagrangian and Eulerian mesh formulations. 

The analyses are applied to examine the structural behavior of 

railroad tank cars under a generalized head impact scenario. 

Structural behavior is calculated in terms of forces, 

deformations, and puncture resistance. Results from the two 

finite element codes are compared to verify this methodology 

for head impacts. In addition, FEA results are compared to 

those from a semi-empirical method. 

INTRODUCTION 

Recent train derailments involving the release of 

hazardous materials (hazmat) have prompted renewed focus 

on the structural integrity of tank cars during accidents [1-3]. 

Consequently, the industry began efforts to develop improved 

designs while the government initiated research to develop 

performance standards for tank cars carrying hazmat [4]. 

The Volpe National Transportation Systems Center (Volpe 

Center) provides technical support to the Federal Railroad 

Administration (FRA) by conducting and managing research 

to evaluate the structural integrity and crashworthiness of tank 

cars carrying hazmat. Prior to these recent accidents, the 

objective of FRA/Volpe Center research was to maintain tank 

integrity under normal operating conditions (e.g., metal 

fatigue and damage tolerance). More recently, the focus of the 

research has shifted to also maintain tank integrity under rare 

and extreme circumstances such as impact loading during 

accidents. Previous research has been conducted by the Volpe 

Center to examine tank car impacts to the head [5] and the 

side or shell [6, 7] of tank cars. Such failures occur from 

collisions with objects such as couplers and wheels from 

adjacent cars, broken rails, etc. 

In the 1970s, a semi-empirical method to examine tank 

car head puncture was developed through the Railroad Tank 

Car Safety Research and Test Project [8].1

 This method 

included equations to calculate puncture velocity, which is the 

impact velocity at which puncture of the commodity tank is 

expected to occur. Subsequently the semi-empirical method 

was modified to account for the presence of jackets and head 

shields [9]. Correlations with data from additional sources 

[10] and with engineering analyses [11] indicate that the semiempirical approach to predict puncture velocity gives 

reasonable but conservative estimates. That is, puncture is 

expected to occur at velocities greater than the calculated 

value. 

FEA offers an alternative approach to the semi-empirical 

approach, which can reduce conservatism since it provides 

more realistic modeling of impacts. Results from FEA models 

were presented previously in reference [5], but the effects of 

 

1

 This project is now co-sponsored by the Railway Supply Institute (RSI) and 

the Association of American Railroads (AAR). 
This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

2 

fluid-structure interaction and material failure were not 

included. Over time, the capabilities of state-of-the-art FEA 

software have progressed to readily implement these effects. 

A methodology using commercial FEA software was recently 

developed to examine shell impacts accounting for fluidstructure interaction and material failure. In this paper, the 

FEA methodology for shell impacts is adapted to examine 

head impacts in a consistent and analogous manner. 

This paper describes dynamic, nonlinear finite element 

models to examine the structural behavior of tank cars under a 

generalized head impact scenario. These models were 

developed using commercial finite element codes ABAQUS 

[12] and LS-DYNA [13], which were used previously in the 

methodology developed for shell impacts. Structural behavior 

is examined in terms of impact force as a function of 

indentation. Force-indentation characteristics are examined 

for different tank car configurations. These configurations 

include a baseline conventional tank car designed to carry 

liquid chlorine, a baseline tank with a head shield, and a 

baseline tank with increased thickness and a head shield. In 

addition, puncture velocities are calculated for these different 

configurations. FEA results are compared to those from the 

semi-empirical method. 

Confidence and credibility in the FEA models for shell 

impacts was achieved through a process of verification and 

validation.2

 Verification was conducted by comparing results 

from both solvers with each other and with known solutions 

for static loading. Validation for shell impacts was 

accomplished through comparisons with data obtained from 

full-scale tests that were performed at the Transportation 

Technology Center in Pueblo, Colorado [6]. In this paper, 

verification of the FEA models for generalized head impacts is 

conducted by comparing results from both solvers with each 

other. 

FINITE ELEMENT ANALYSIS 

Finite element models are developed to examine the 

deformation and failure of railroad tank cars due to head 

impacts. The idealized impact scenario is a tank car moving 

into a fixed and rigid indenter at a given impact velocity. 

Figure 1 shows a schematic of the FEA model for the 

idealized head impact scenario. The impact location on the 

tank head is 34 inches below the center of the head. Unless 

specified otherwise, the dimensions of the indenter face are 6 

inches by 6 inches with 0.5-inch edge radii. 

All tank cars models are half-symmetric about the 

longitudinal center plane with 10.6 percent outage3

 and an 

internal pressure of 100 psi. The elliptical shape of the end 

caps is created with an aspect ratio of 2. An 11-gage (0.119-

 

2

 In the present context, verification refers to the process in ensuring that the 

mathematics are being modeled correctly. Validation refers to the process in 

determining whether physics are being modeled correctly [14]. 

3

 Outage is the unfilled volume of the tank. Therefore 10.6 percent outage 

represents a tank that is slightly less tan 90 percent full. 

inch thick) jacket is modeled with a 4-inch separation to 

account for the presence of insulation and thermal protection 

between the commodity tank and the jacket. 

The FEA models do not include tank car components 

such as the manway, body bolsters, draft sills, and safety 

appliances. Despite these simplifications, the computational 

times for the FEA models are extensive because the models 

account for the following physical characteristics of 

deformable bodies under impact loading: (1) structural 

dynamics, (2) elastic-plastic material behavior with large 

deformations, (3) fluid-structure interaction, and (4) material 

failure. 

FEA is well established as a computational tool to model 

structural dynamics to simulate structure movement with 

respect to time under prescribed loads. 

Both ABAQUS and LS-DYNA include standard 

constitutive models for elastic-plastic stress-strain behavior 

with large deformation. The elastic-plastic material behavior 

is modeled using Ramberg-Osgood equation for strain as a 

function of stress. 

n

E K

σ σ

ε = + ⎛ ⎞ ⎜ ⎟ ⎝ ⎠ (1) 

where ε is the strain, σ is the stress, n and K are material 

constants and E is the modulus of elasticity. Table 1 lists 

constants and mechanical properties of the tank car steels that 

are used in the FEA models described in this paper. In current 

tank car construction, the commodity tank is nominally made 

with normalized TC-128B steel. The properties listed in the 

table for TC-128B correspond to tensile measurements 

performed on tank car that punctured in a full-scale shell 

impact test [6]. Outer jackets are typically made with A1011 

steel. Properties for A1011 are available from the Internet. 

Current practice requires that commodity tanks greater than 1 

inch thick must be built with steels other than TC-128B. In 

these cases, A516-70 steel is used in the FEA models. The 

properties listed for this particular steel are obtained from 

reference [15]. 

Figure 1: Schematic of FEA Simulation 

Jacket Tank 

Fixed Indenter Moving Direction of Tank Car 
This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

3 

Table 1: FEM Constants and Mechanical Properties 

 TC-128B A1011 A516-70 

Modulus of elasticity, E (ksi) 31,650 29,000 30,000 

Hardening exponent, n 11.17 9.00 10.64 

R-O Constant, K (ksi) 96.04 59.85 89.69 

Yield strength (ksi) 55.05 30 50 

Tensile strength (ksi) 83.05 50 70 

When there is fluid inside the tank, both the fluid and the 

tank move and exert forces upon one another during impact. 

Different mesh representations are used in the FEA models to 

account for this fluid-structure interaction behavior. 

Specifically, Lagrangian and Eulerian mesh formulations are 

used. In the Lagrangian fluid formulation, the nodes of the 

mesh representing the fluid follow the material of the structure 

as it deforms. This formulation is used in both the ABAQUS 

and LS-DYNA simulations discussed in this paper. An 

Eulerian mesh is fixed in space and tracks the material 

movement inside the structural Lagrangian mesh of the tank. 

The Eulerian formulation is implemented using LS-DYNA. 

Previous research on tank car shell impacts [6, 7] indicated 

that the Eulerian mesh provided a more accurate 

representation of fluid-structure interaction than the 

Lagrangian mesh when compared to test data. 

ABAQUS Implementation

The ABAQUS simulations discussed in this paper are 

performed with the explicit dynamics program 

ABAQUS/Explicit Version 6.7-1 [12]. 

The tank car assembly of the ABAQUS model includes 

the deformable tank, jacket and fluid components. Two planar 

rigid bodies are also placed in front and rear positions under 

the tank car assembly to simulate some effects of rail car 

wheels. These front and rear “wheels” are coupled in rigid 

body motion with selected front and rear element sets, 

respectively, in the bottom of the tank car assembly. A rigid 

“floor” prevents the “wheels,” as well as the tank car 

assembly, from moving downward. The tank car assembly 

and the “wheels” are assigned an initial horizontal speed 

toward a rigid indenter that is constrained in all degrees of 

freedom. 

Shell elements used in conjunction with elastic-plastic 

constitutive relations are accurate and efficient in simulating 

the force-deformation behavior of the tank structure without 

failure. In modeling failure, however, solid elements in the 

vicinity of impact are needed to produce accurate results in 

simulating progressive damage and fracture behavior. A small 

sub-domain at and around the location of impact is modeled 

with solid elements, whereas the remaining tank structure is 

modeled with shell elements. This computational strategy is 

implemented using the solid-to-shell coupling capability 

within ABAQUS [12]. Figure 2 shows a typical solid-to-shell 

coupling mesh in the model. 

Figure 2: Close-Up View of a Typical Solid-to-Shell 

Coupling Mesh 

Material failure is implemented in ABAQUS with a 

standard constitutive material model and a resident failure 

initiation and progression model based on the general state of 

stress and strain softening. Failure is assumed to initiate when 

loading conditions induce effective plastic strains above a 

threshold value that depends on the general state of stress in 

terms of a quantity called stress triaxiality. Stress triaxiality is 

the ratio of mean stress to the effective or von Mises 

equivalent stress. Figure 3 shows a schematic of the effective 

plastic strain to initiate failure, εi as a function of stress 

triaxiality, η. Moreover, this envelope is referred to as the 

Bao-Wierzbicki (B-W) criterion [16]. The schematic indicates 

that the B-W failure initiation envelope consists of three 

regions, each representing a different mode of failure. Region 

I consists of high positive values of stress triaxiality which 

promotes nucleation, growth, and coalescence of voids 

leading to ductile fracture. Region III consists of negative 

values of stress triaxiality which represent shear fracture due 

to shear band localization. Region II comprises positive but 

low values of stress triaxiality, and represents mixed fracture. 

Once failure initiates, damage is assumed to progress in 

the form of strain softening. The resident failure model in 

ABAQUS has the option to specify linear or exponential 

strain softening. In the present implementation, linear strain 

softening is assumed. Figure 4 illustrates this concept in 

which the stress-strain behavior of a material element exhibits 

a linear decrease in stress with increasing strain beyond εi. 

The implementation of progressive damage in ABAQUS is 

actually in the form of a stress-displacement where the 

effective plastic strain is multiplied by a characteristic length.4

 

 

4

 For shell and two-dimensional elements, this characteristic length is the 

square root of the integration point area; for three-dimensional elements, it is 

the cube root of the integration point volume. The definition of the 

characteristic length indicates that some mesh dependency is expected when 

elements have poor aspect ratios. 
This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

4 

Figure 3: Schematic of Fracture Initiation Envelope 

Based on Stress Triaxiality 

Figure 4: Schematic of Linear Strain Softening 

The ABAQUS implementation of the B-W criterion was 

used to calculate the energy to fracture unnotched Charpy 

specimens made from TC-128B tank car steel under pendulum 

impact loading [17]. Results from the FEA simulations were 

in excellent agreement with the experimental data for the 

range of specimen thicknesses that were tested. Subsequently, 

this material failure methodology was used in conjunction 

with a Lagrangian fluid mesh formulation to predict puncture 

in a full-scale tank car shell impact test [6]. 

LS-DYNA Implementation

The finite element models used in the LS-DYNA 

simulations are developed using Altair’s software Hypermesh. 

All LS-DYNA simulations discussed in this paper are 

performed with Livermore Software Technology 

Corporation’s (LSTC) LS-DYNA3D (version 970) [13], an 

explicit finite element solver for modeling impact. 

The tank car container and jacket structure are modeled 

using shell elements. To minimize computational time, the 

FEA model of the tank consists of two parts: (1) a large area 

of rigid material away from the impacting end and, (2) a 

smaller area of deformable material at the impacting end, as 

illustrated in Figure 5. The model has boundary conditions 

similar to those used in ABAQUS simulations. Both Eulerian 

and Lagrangian fluid formulations are used in the modeling of 

fluid in LS-DYNA simulations. 

Figure 5: LS-DYNA Model of Rigid-Deformable Tank 

The LS-DYNA FEA model with fluid-structure 

interaction uses Arbitrary-Lagrangian-Eulerian (ALE) 

coupling, which consists of four parts: (1) the tank structure 

(Lagrangian mesh), (2) an air block surrounding the tank 

structure (Eulerian mesh), (3) the liquid inside the tank 

(Eulerian mesh), and (4) the vapor outage that fills the 

remaining volume inside the tank (Eulerian mesh). In this 

context, a Lagrangian mesh is one that transforms according 

to its deformation; an Eulerian mesh is fixed in space through 

which material flows. 

Material deformation for the fluid is characterized by a 

constitutive model called MAT_NULL with an equation of 

state, with a density of 0.051048 lbs/in3

 and bulk modulus of 

2.25 psi. 

At present, LS-DYNA does not have a resident material 

model to implement the failure criterion described previously. 

Implementation of the B-W criterion can be performed 

through the user-defined material capability in LS-DYNA, but 

was conducted in this paper. 

FEA RESULTS 

The FEA models developed for railroad tank car head 

impacts are used to: (1) compare results from the two solvers 

with different formulations to account for fluid-structure 

interaction, (2) examine force-indentation behavior of 

different tank car configurations, and (3) predict puncture. 

Rigid Parts 

Deformable Parts 
This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

5 

Comparison of Solvers and Fluid Formulations

Fluid-structure interaction is modeled in LS-DYNA using 

either a Lagrangian or an Eulerian mesh for the fluid. In 

ABAQUS, the fluid is modeled with a Lagrangian mesh. In 

both solvers, the tank structure is modeled with a Lagrangian 

mesh. In the previous work on tank car shell impacts [6], the 

LS-DYNA implementation of the Eulerian fluid provided 

excellent agreement with full-scale impact test data. 

FEA results from ABAQUS and LS-DYNA with different 

fluid mesh formulations are shown in Figure 6. The tank car 

is traveling at 10 miles per hour (mph) in these simulations. 

The maximum impact forces are within 10 percent. 

Furthermore, these results show that there is no significant 

difference among the three models during the initial 0.05 

second. 

Figure 7 illustrates the corresponding force-indentation 

characteristics for these simulations. Indentation is measured 

from the initial position of the commodity tank. The figure 

indicates that all of the models are generally in good 

agreement, specifically the two models based on the 

Lagrangian fluid formulation. Differences are evident in the 

unloading portion of these curves that characterize the 

permanent deformation of the tank. However, the differences 

in permanent indentations are also within 10 percent. 

Maximum indentations are within 10 percent of each other. 

Structural Response of Different Configurations

The force-indentation behavior of different tank car 

configurations is examined using LS-DYNA with an Eulerian 

mesh representing the fluid content inside the tank. The 

combination of LS-DYNA and Eulerian fluid mesh is chosen 

because the previous results with different solvers and fluid 

meshes showed no significant differences. In addition, the 

previous work using LS-DYNA with the Eulerian fluid mesh 

agreed well with full-scale shell impact test data [6]. 

Table 2 lists the three configurations considered in this 

paper. In general, the variables in these configurations are 

tank thickness, jacket thickness, and material (i.e., steel 

specification). In the configurations with head shields, the 

jacket in the head is replaced with a thicker sheet made of 

different steel. Varying these thicknesses also changes the 

gross weight of the tank car. 

Figure 8 compares the force-time histories for these 

simulations. The peak impact forces increase as the tank head 

is thickened and head protection is added. The variation in 

peak forces among the three cases is approximately 20 

percent. 

Figure 9 shows the corresponding force-indentation 

curves. These curves have a nearly bi-linear character with a 

slightly higher breakpoint as additional layers of steel are 

added to the entire structure. This figure also indicates that 

adding thickness to the tank and providing a head shield 

decreases maximum indentation by as much as 23 percent. 

Time (seconds)

0.00 0.02 0.04 0.06 0.08 0.10 0.12 0.14

Force (kips)

0

200

400

600

800

1000

ABAQUS, Lagrangian Fluid

LS-DYNA, Lagrangian Fluid

LS-DYNA, Eulerian Fluid

Figure 6: Force-Time Histories for Head Impact 

Simulations at 10 mph 

Indentation (inches)

0 1 2 3 4 5 6 7 8 9 10

Force (kips)

0

200

400

600

800

1000

ABAQUS, Lagrangian Fluid

LS-DYNA, Lagrangian Fluid

LS-DYNA, Eulerian Fluid

Figure 7: Force-Indentation Curves for Head Impact 

Simulations at 10 mph 

Table 2: Characteristics of Tank Car Configurations 

 Configuration 1 2 3 

Characteristic 

Baseline Baseline 

with 

Head Shield 

Thicker 

Baseline 

with 

Head Shield 

Inner Diameter (inch) 100.625 100.625 100.625 

Weight (lb) 266,000 268,000 275,000 

Tank Head Thickness (inch) 0.828 0.828 1.108 

Tank Material TC-128B TC-128B A516-70 

Tank Shell Thickness (inch) 0.777 0.777 0.932 

Tank Shell Material TC-128B TC-128B TC-128B 

Jacket Head Thickness (inch) 0.119 0.5 0.5 

Jacket Head Material A1011 A516-70 A516-70 

Jacket Shell Thickness (inch) 0.119 0.119 0.119 

Jacket Shell Material A1011 A1011 A1011 

Outage 10.6% 10.6% 10.6% 

Internal Pressure (psi) 100 100 100 
This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

6 

Time (seconds)

0.00 0.02 0.04 0.06 0.08 0.10 0.12 0.14

Force (kips)

0

200

400

600

800

1000

1200

Thicker Baseline with Head Shield

Baseline with Head Shield

Baseline

Figure 8: Simulated Force-Time Histories for 10-mph 

Head Impacts on Different Configurations 

Indentation (inches)

0 2 4 6 8 10

Force (kips)

0

200

400

600

800

1000

1200

Thicker Baseline with Head Shield

Baseline with Head Shield

Baseline

Figure 9: Simulated Force-Indentation Curves 10-mph 

Head Impacts on Different Configurations 

The force-indentation behavior of different configurations 

is examined further by varying the impact speed. Table 3 

compares the maximum forces for the different tank car 

configurations at three impact speeds between 10 and 15 mph. 

The numbers in parentheses refer to results from the semiempirical method to calculate impact force as a function of 

velocity. Forces calculated with the semi-empirical method 

are generally higher than those from the FEA model. The one 

exception is the thicker baseline with head shield at 10 mph 

where the semi-empirical result is about 3 percent lower than 

the FEA calculation. Otherwise the semi-empirical results are 

between 7 and 33 percent higher than the FEA results. The 

differences in peak forces between the two methods become 

larger as impact velocity increases. 

Table 3: Comparison of Maximum Force for Different 

Impact Speeds (kips) 

Speed of Moving 

Tank Car 

Configuration 

10 mph 12.5 mph 15 mph 

Baseline 813 

(905) 

984 

(1265) 

1248 

(1663) 

Baseline with Head Shield 857 

(916) 

1132 

(1280) 

1412 

(1682) 

Baseline with Increase 

Thickness and Head Shield 

982 

(952) 

1254 

(1330) 

1562 

(1748) 

The impact scenario for which the semi-empirical method 

was developed is a moving ram car striking the head of a 

subject tank car below the centerline of the head. The impact 

location is assumed to be halfway between the centerline of 

the head and the bottom of the tank. The subject tank car with 

brakes released is braced by three fully-loaded backup or anvil 

cars with their brakes applied. Moreover, the generalized 

impact scenario examined by FEA in this paper is considered 

more severe than the one developed for the semi-empirical 

method. The equations comprising the semi-empirical method 

to calculate force, indentation, and puncture velocity for head 

impacts were originally reported in reference [8]. The 

modifications to include the presence of jackets and head 

shield are listed in reference [9]. In addition, the semiempirical equations may also be found in reference [10]. 

Table 4 compares maximum indentations from the FEA 

simulations and the semi-empirical method. These results 

indicate that thickening the commodity tank and providing a 

head shield reduce maximum indentation. The table also 

indicates that the semi-empirical approach calculates 

maximum indentations that are between 40 and 70 percent less 

than those from the finite element method. 

Table 4: Comparison of Maximum Indentation for 

Different Impact Speeds (inches) 

Speed of Moving 

Tank Car 

Configuration 

10 mph 12.5 mph 15 mph 

Baseline 8.6 

(5.1) 

10.8 

(6.4) 

12.9 

(7.7) 

Baseline with Head Shield 7.6 

(3.1) 

10.0 

(3.9) 

12.0 

(4.6) 

Baseline with Increase 

Thickness and Head Shield 

6.6 

(2.1) 

9.0 

(2.6) 

11.1 

(3.2) 

Comparisons between the finite element and semiempirical results show the conservative nature of the semiempirical approach. However, while the semi-empirical 

method can provide reasonable estimates of peak impact force 

in some cases, it significantly underestimates maximum 
This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

7 

indentation. The discrepancies between results from the FEA 

and the semi-empirical method may be attributed to 

differences in theoretical bases. The theoretical basis for the 

semi-empirical method is Hertz contact, which assumes quasistatic, elastic deformation of bodies in contact. Collisions that 

occur during accidents are likely to create permanent plastic 

deformations for which Hertz contact theory is not applicable. 

Tank Car Head Puncture Predictions

Under relatively low initial impact velocities, the 

commodity tank may be permanently deformed but not 

punctured. As the impact velocity increases, the likelihood of 

puncture and consequent loss of structural integrity becomes 

greater. Therefore, a minimum initial impact velocity exists 

that first leads to puncture, which can be defined as a 

threshold puncture velocity. This threshold puncture velocity 

depends on factors such as impact mass, material, geometric 

and connectivity configurations of the tank car assembly 

(including type and outage amount of any fluid content), 

shape, size and location of the indenter, and all relevant initial 

and boundary conditions. 

The ABAQUS model is exercised to predict puncture of 

railroad tank cars under head impacts. Particular focus is 

given to examine the effects of tank car thickness and indenter 

size. The three tank car configurations outlined in Table 2 are 

considered. Increased tank thicknesses in Configurations 2 

and 3 lead to slightly higher collision mass compared to the 

Configuration 1. Being consistent with industrial 

applications, these two configurations also have different tank 

car steel materials in the head and/or the head jacket. The 

effect of indenter size is studied by considering both a 6-inch 

by 6-inch and a 12-inch by 12-inch indenter with a squareshaped face. The locations of the indenter centers relative to 

the tank car assembly are identical in the case studies. 

The three tank car configurations and the two indenter 

sizes yield a maximum of six combinations for case studies. 

The model is exercised for five combinations without the 

combination of Configuration 3 and the larger size indenter. 

For each combination under consideration, finite element 

analyses incorporating the progressive damage and failure 

material models are conducted for initial impact velocities 

incremented at 1 mph. From the analyses, two impact 

velocities can be identified for each combination: (1) the 

highest velocity under which puncture is not clearly present 

(vnp), and (2) the lowest velocity under which puncture is 

clearly observed (vp). The estimated threshold puncture 

velocities clearly lie between these two characteristic 

velocities. 

Figure 10 shows four possible states of damage in the 

impacted region that develop on the commodity tank in the 

simulations, which help determine vnp and vp. State (a) shows 

a permanently dented tank with surface damage. State (b) 

shows a more severely damaged tank where the local 

thickness has reduced significantly but shows no evidence of 

through-the-thickness damage. State (c) shows obvious 

damage through the thickness. Finally, state (d) shows full 

penetration or puncture with or without turning part of the 

tank into a flap. Generally, vnp corresponds to initial impact 

velocities that lead to damage states (a) or (b), and vp to those 

that lead to damage states (c) and (d). Special considerations 

are made for initial impact velocities leading to damage states 

(b) and (c) since these velocities appear to be extremely close 

to the threshold puncture velocity. For example, when vnp is 

determined according to damage state (b), the corresponding 

vp is denoted as vnp+. When vp is determined according to 

damage state (c), the corresponding vnp is denoted as vp-. 

The vnp and vp results are tabulated in Table 5 for all five 

combinations denoted as Cases A through E. Identifying and 

categorizing damage states, particularly (b) and (c), can be 

subjective. Consequently, some numbers listed in Table 5 are 

changeable within their close neighborhoods. The table also 

includes predictions for puncture velocity based on the semiempirical method. In general, the puncture velocities from the 

semi-empirical methods are less than those from the FEA for 

the same configuration and indenter size. Moreover, Table 5 

indicates that increased tank car thicknesses and adding a head 

shield provide marginal or incremental improvements in the 

estimated threshold puncture velocities, and indenter size has 

a significant effect on the estimated puncture velocity. 

Figure 10: Potential Damage States of Impacted Region 

on Commodity Tank 
This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

8 

Table 5: Puncture Velocity Estimation 

FEA SemiEmpirical Case Configuration / 

Indenter size vnp

(mph) 

vp 

(mph) 

vp 

(mph)

A Configuration 1 / 

6-inch indenter 9 10 8.9 

B Configuration 2 / 

6-inch indenter 10 11 10.3 

C Configuration 3 / 

6-inch indenter 11 12 10.5 

D Configuration 1 / 

12-inch indenter 16 16+ 14.0 

E Configuration 2 / 

12-inch indenter 16 17 16.3 

Figure 11 shows the force-indentation curves obtained 

from the analyses for the five combinations, denoted as Cases 

A through E. The curve for each combination corresponds to 

an initial impact velocity that is closest to the estimated 

threshold puncture velocity. As shown in previous results, 

thickening the tank and providing a head shield tends to 

increase the impact force. Cases A and D correspond to the 

baseline tank car configuration with two indenter sizes. 

Similarly, Cases B and E correspond to the configuration for a 

baseline tank with head shield and different indenters. In both 

configurations, the force levels for the larger indenter are 

higher than those for the smaller indenter. For a given 

configuration, higher force levels associated with higher 

impact speeds are needed to puncture the tank with a larger 

indenter. In terms of energy to puncture, which is the area 

under the force-indentation curve, the larger indenter requires 

substantially more energy to puncture than the smaller 

indenter. 

Indentation (inches)

0 2 4 6 8 10 12 14 16 18

Force (kips)

0

200

400

600

800

1000

1200

1400

1600

Case A: 10 mph

Case B: 11 mph

Case C: 12 mph

Case D: 16 mph

Case E: 17 mph

Figure 11: Force-Indentation Curves from Puncture 

Study 

CONCLUDING REMARKS 

Dynamic, nonlinear (i.e., elastic-plastic) finite element 

models have been developed to study the force-indentation 

behavior of railroad tank cars under head impact conditions. 

The models were developed using two commercial finite 

element codes, ABAQUS and LS-DYNA. These codes were 

used previously to develop a finite element framework to 

examine the structural behavior of tank cars under shell 

impacts [6, 7]. In this paper, the FEA framework was adapted 

to address head impacts in a consistent and analogous manner 

like shell impacts. 

Different fluid mesh formulations were used to account 

for the effect of fluid-structure interaction in the FEA models. 

The models with different fluid mesh formulations were 

generally in agreement with each other. 

The FEA models for head impacts were used to examine 

force-indentation behavior of different tank car 

configurations. These models showed that increasing the 

thickness of the head and adding a head shield tend to increase 

the maximum impact force while decreasing the maximum 

indentation. 

Results from the FEA models for head impacts were 

compared to those from a semi-empirical method originally 

developed in the 1970s and subsequently modified to account 

for the presence of jackets and head shields. Peak impacts 

forces estimated from the semi-empirical method were 

generally higher than those from FEA. Conversely, maximum 

indentations calculated from the semi-empirical method were 

significantly less than those from FEA. Moreover, the 

comparisons suggest that the semi-empirical method provides 

reasonable but conservative estimates for peak impact force. 

Estimates for maximum indentation based on the semiempirical method are significantly less than those from the 

FEA models. 

The FEA models were also used to predict puncture of the 

tank car head. The results presented in this paper indicate that 

increasing the head thickness and adding a head shield 

provide marginal or incremental improvements in puncture 

velocity. The semi-empirical method generally predicts lower 

puncture velocities than the finite element method. The 

results also suggest that indenter size has a significant effect 

on the estimated puncture velocity. Moreover, the results 

presented in this paper are qualitatively and quantitatively 

consistent with FEA results previously conducted for shell 

impacts [7]. 

ACKNOWLEDGMENTS 

The Federal Railroad Administration (FRA) Office of 

Research & Development sponsored the work described in 

this paper. Mr. Francisco Gonzalez is the FRA project 

manager for research on railroad tank cars. Mr. Eloy Martinez 

also provided technical direction to this project. Technical 

discussions with Professor A. Benjamin Perlman of the Volpe 

Center are greatly appreciated. Finally, the authors would like 
This material is declared a work of the U.S. Government and is not subject to copyright protection in the United States. Approved for 

public release; distribution is unlimited. 

9 

to acknowledge Professor Christopher Barkan of the 

University of Illinois at Urbana-Champaign for his assistance 

in providing the Volpe Center with access to computers at the 

National Center for Supercomputing Applications. 

REFERENCES 

[1] National Transportation Safety Board, 2004: 

“Derailment of Canadian Pacific Railway Freight Train 

292-16 and Subsequent Release of Anhydrous Ammonia 

Near Minot, North Dakota January 18, 2002,” Railroad 

Accident Report NTSB/RAR-04/01. 

[2] National Transportation Safety Board, 2005: “Collision 

of Norfolk Southern Freight Train 192 With Standing 

Norfolk Southern Local Train P22 With Subsequent 

Hazardous Materials Release at Graniteville, South 

Carolina January 6, 2005,” Railroad Accident Report 

NTSB/RAR-05/04. 

[3] National Transportation Safety Board, 2006: “Collision 

of Union Pacific Railroad Train MHOTU-23 With BNSF 

Railway Company Train MEAP-TUL-126-D With 

Subsequent Derailment and Hazardous Materials 

Release, Macdona, Texas, June 28, 2004,” Railroad 

Accident Report NTSB/RAR-06/03. 

[4] Tyrell, D.C., Jeong, D.Y., Jacobsen, K., Martinez, E., 

2007: “Improved Tank Car Safety Research,” 

Proceedings of 2007 ASME Rail Transportation Division 

Fall Technical Conference, RTDF2007-46013. 

[5] Jeong, D.Y., Tang, Y.H., Yu, H., Perlman, A.B., 2006: 

“Engineering Analyses for Railroad Tank Car Head 

Puncture,” Proceedings of IMECE2006, 2006 ASEM 

International Mechanical Engineering Congress and 

Exposition, IMECE2006-13212. 

[6] Tang, Y.H., Yu, H., Gordon, J.E., Priante, M., Jeong, 

D.Y., Tyrell, D.C., Perlman, A.B., 2007: “Analysis of 

Full-Scale Tank Car Shell Impact Tests,” Proceedings of 

2007 ASME Rail Transportation Division Fall Technical 

Conference, RTDF2007-46010. 

[7] Tang, Y.H., Yu, H., Gordon, J.E., Jeong, D.Y., 2008: 

“Analysis of Railroad Tank Car Shell Impacts Using 

Finite Element Method,” Proceedings of the 2008 

IEEE/ASME Joint Rail Conference, JRC2008-63014. 

[8] Shang, J.C., Everett, J.E., 1972: “Impact Vulnerability 

of Tank Car Heads,” Shock and Vibration Bulletin 42, 

197-210. 

[9] Belport, S.M., 1993: “Evaluation of the Puncture 

Resistance of Stainless Steel and Carbon Steel Tank 

Heads,” AAR Report No. P-93-114. 

[10] Jeong, D.Y., Tang, Y.H., Perlman, A.B., 2001: 

“Evaluation of Semi-Empirical Analyses for Railroad 

Tank Car Puncture Velocity, Part I: Correlations with 

Experimental Data,” Volpe Center Report, 

DOT/FRA/ORD-01/21.1. 

[11] Jeong, D.Y., Tang, Y.H., Perlman, A.B., 2001: 

“Evaluation of Semi-Empirical Analyses for Railroad 

Tank Car Puncture Velocity, Part II: Comparisons with 

Engineering Analyses,” Volpe Center Report, 

DOT/FRA/ORD-01/21.2. 

[12] ABAQUS User’s Manual, Hibbit, Karlsson & Sorensen 

Inc., Pawtucket, Rhode Island. 

[13] LS-DYNA3D User’s Manual, Version 970, Livermore 

Software Technology Company, Livermore, California. 

[14] American Society of Mechanical Engineers, 2006: 

“Guide for Verification and Validation in Computational 

Solid Mechanics,” ASME V&V 10-2006, New York, 

NY. 

[15] Joia, C.J.B, Carneval, R.O., Soares, S.D., Bezerra, 

P.S.A., Azevedo, C., Cardoso, E.M., Mattos, O.R., 

Menendez, C.M.., 2000: “Monitoring hydrogen damage 

in pipelines and pressure vessels,” Corrosion 2000, 

Paper No. 469, NACE International, Houston, Texas. 

[16] Bao, Y., Wierzbicki, T., 2004: “On fracture locus in the 

equivalent strain and stress triaxiality space,” 

International Journal of Mechanical Sciences 46, 81-98. 

[17] Yu, H., Jeong, D.Y., Gordon, J.E., Tang, Y.H., 2007: 

“Analysis of Impact Energy to Fracture Unnotched 

Charpy Specimens Made from Railroad Tank Car Steel,” 

Proceedings of the 2007 ASME Rail Transportation 

Division Fall Technical Conference, RDTF2007-46038.